Understanding stress analysis limitations

[chipwitch]

I know Inventor's integrated analysis environments are not comprehensive.  I also know that it's commonly said that the built-in stress analysis environment isn't capable of accurately analyzing the simple clevis pin.

I've attached a screen shot of a model of a clevis link with a pin in either end.  I would find it very helpful if someone well-versed in FEA could help me, a noob, understand where the attached image falls short?  In other words, why is it wrong?  Is there anything of value that can be drawn from the analysis?

To my untrained eye, the image appears to be somewhat accurate qualitatively.  Are the innacuracies to be expected more on the quantitiative side of things?

[vex]

I'll take a gander at this...

I'm not 100% sure what you are referring too when you say the FEA in Inventor isn't accurate... it's about as accurate as you make it.  Sure there's things it simply can not do, but for 90% of most structural analysis, it does good enough.  The points where it falls short are more along the lines of discrete control of the mesh generation (IE, you can't generate mesh by hand, dictating the vertices and then the connecting lines, etc), but there are ways to make Inventor get around that.  Some other parts where it falls short is analysis in the plastic deformation/non-linear area of the materials and thermal loading analysis.  Which is to be expected. For the other 90%, as I said before, it does good enough.

I'm a bit confused by your setup you show in your picture.  You show two sets of forces acting, in what appears to be, equal and opposite directions (that's mostly an assumption on my part).  First, have you fixed or pinned any part of your geometry?  It doesn't look like it to me, so that means that any instability or offset in the forces may, infact, cause a large displacment without an applicable stress/strain applied (a source of inaccuracy).  This also will play in to your convergence criterion.  I would suggest first isolating the main part you wish to analyze.  Namely the connecting geometry between the two pins.  You can then fix or pin one hole in your geometry (fixing it in the coordinate system is important).  You then can apply the required force acting in the required direction in the other hole (remote force should work fine).  Remember the application of forces is a little different in Inventor and is based on the number of faces you select and their respective areas.  For this analysis, so long as you don't get into the plastic deformation/non-linear deforming areas it should be fine.  You'll get some amount of stress singularities where the mesh refinement would necessitate infinate number of elements (sharp corners, constraints, etc).

I would highly recommend working through a few cases or tutorials to confirm what you think may be an inaccuracy with the tool.  Just remember, junk in = junk out.  No amount of pretty colors will obviate that.

[chipwitch]

The lack of accuracy to which I was referring is with respect to the "clevis pin problem."  I thought that would be clear enough as I've seen it discussed pretty extensively in one form or another.  Specifically, it is the problem of modeling the interraction between two cylindrical surfaces where one resides inside the other... a bearing surface.  Inventor's FEA is not designed to accurately analyze these surfaces.  These surfaces, at the point of contact, require more intense analysis as you have a line of contact rather than two surfaces.  The greater the disparity in diameters between the two joined parts, the greater the error the integrated FEA will introduce.  My understanding is because it doesn't take into account the deformation of the mating surfaces that ultimately happen in the real world.

Yes, I have loads in opposite directions to obtain equilibrium.  I realize this is a bit convoluted, but the result shouldn't be affected, I wouldn't think.  Normally I would fix a surface and in fact have pinned one of the pins.  This model I came at from the Dynamic analysis approach.  When I began customizing contacts and loads, this was the result.  I have no aversion to doing it via a fixed surface or pin.  It was just an experiment.  It would be wrong to conclude that because someone doesn't understand something that they hadn't already gone through numerous tutorials.  I didn't start my quest for knowledge in a forum.

So, the problem I'm having is specifically with contact types, when to use which one and how the results are affected by ones choice.  I'm not 100% certain in the case of the pin/clevis which contact to use.  Is the sliding/no separation correct?

[vex · Accepted solution]

Forgive this piecemeal response.  I appreciate the explination of the "cleavis pin problem" as you've described it.  Unfortunately I have not seen any other discussions of it through my quick google search.  Based on your explination it sounds like a standard stress singularity problem (a requirement for additional mesh geometry to be applied to an infinitely small area--This is why the simulation is only converged on the displacement feature).  To illustrate the issue I did a quick analysis that has a good example of it.  Although not exactly referencing the pin portion of the problem it does illustrate the mesh refinement and the increased stresses at the sharp corner (an infinetely small area).  As you can see I simpilified the model by cutting it in half and holding the cut portion of it in a fixed manner.  You can pull resultant forces by right clicking on the constraints.  I also applied one force, acting equally on the bearing surfaces.  If I wish to have it act on a smaller surface I can split the surface into a smaller area.  In real life the plastic deformation of the pin will automatically increase the surface of action.  Making the simiplifying assumption that the area is significant and translates the majority of the force through the part would decrease the requirements imposed by the stress singularities.

I've included another quick simulation where I split the surface and applied the same load to those smaller faces (increasing the local stress due to the 200 lb load acting on a roughly 0.5 in^2 face).  I would have included the opposite shot of the sharp corner, but I'm only allowed to upload 3 things per post :(.  In any case, there was no mesh refinement at that location as the stress applied to the pin holes was where the peak stress should occur.  This also allowed the stress to converge relatively quickly.  As the area of action is reduced (the pin and hole interface) the higher the stress concentration will be until you begin to get into the plastic deformation of the stress-strain curve.  As I said in my first post, Inventor does a fine job for 90% of things.  As soon as you start getting into the plastic deformation of the material, it's no longer accurate.

Going through the Assembly side of things you'll run into the same issue.  So long as you are not approaching yield of the material, and your constraints are setup appropriately, I do not see an issue with the analysis. As your pin diameter decreases relative to the hole size you will get stress singularities, and should be accounted for depending on how and why you're running the analysis.

As for the pin constraints it's going to depend a lot on your application and what you're testing.  If for instance you desire to test a pin, for all intents and puposes, is a face to face contact (slip fit, etc) then I would treat them as equal diameter and just do a contact no slip.  If it's a smaller diameter with a contact, but with slip I would apply that contact.  If you're decreasing the diameter significantly for a failure sort of test, there are ways to do it but you will need to actually alter the material properties of either the pin or cleavis to allow for plastic deformation. IE allowing the compression of the pin into an oblong shape to contact more surface area of the cleavis--or ignore the stress signularities and isolate the portion of the component that is what you are really interested in.

[JDMather]

1. What are you trying to test/analyze?

2. What is the source of your information?

3. Where is your assembly?

[chipwitch]

Thank you for that explanation.  I'm becoming increasingly frustrated by my inability to articulate the problem.  That makes it difficult to google things as well.  You're getting the gist of what I'm after.  I wasn't really thinking about what was going on with the plastic deformation.  I'm not looking for anything complex, like testing the failure of an increasingly smaller pin, as you considered I might.  It's rather simple.  I'm designing a 3-point hitch for a tractor.  If you aren't familiar with it, it's pretty much what it sounds like.  It is a kind of hitch that constrains the farm implement to the tractor essentially in a single unit, transferring the load of the implement through the hitch to the rear wheels rather than simply dragging the implement on the ground.  It can further be described to act much like a 4-bar linkage system in a parallelagram configuration.

I'm wanting to analyze the linkage configuration dynamically so I can see the stresses primarily in the links themselves, with an eye especially on the holes (bearing load) in the links as it is being raised and lowered (usually via hydraulics).  I'm perfectly content with using theoretical equal diameters on the pins and holes.  If this is the ONLY reason the FEA is considered weak, then I should be good to go.  I've been working with Inventor since 2010 and haven't done much with the stress analysis except for some simple parts or welded frames.  I'm just not well versed enough to have the confidence to not screw up the results.  I can see how subjective the results are, even when the data input is valid.  Anyway, because this is a 4-bar linkage (actually a little more complex), I'd like to see the stress on the individual components as it goes through its cycles, dynamically.  Since bearing loads are a significant part of the problem, I was concerned by the warnings I've gotten from others about the lack of accuracy when it comes to the bearing loads.  I even talked to people at Autodesk phone support about this in the past.  It should have occurred to me that the deformation of the parts could ultimately be ignored since the deformation would eventually result in full contact between the parts (in the direction of load). 

With that out of the way... I get what you were illustrating with your models.  While that works just fine for analyzing a single part, two things concern me with respect to my project.  First, it looks like you're applying a "Bearing Load".  That's fine to analyze a single part, but like I intimated, the magnitude and direction of the load will change dynamically.  Second, I'll need to model pins for the joints (?) to do it dynamically as a complete system.  In which case, will they mimic the "Bearing Load"?

Finally, I'm confused on the type of contact you mentioned... "contact no slip."  I don't see any contacts by that name.  When I try any of the other contacts besides the one in the image in the OP, I get entirely different results.  The results in the image seem about right to me?

I appreciate all the time you've taken in your explanation.  It's given me a much better understanding.

[vex]

Sorry about that (my next response will take some time to think out and write), I ment to say slip fit no sliding.  That's a manual contact so there needs to either be a suppressed automatic contact, a manual contact made before you do an automatic, or decrease the size such that the gap is larger than the automatic threshold (or you can adjust the automatic threshold).

As for dynamic simulations, that's a little outside my expertise with Inventor (i've dabbled with it, but not enough to give any advice or direction with).  From my perspective I would treat it as a worst case scenario: you mass*acceleration is going to be your force acting on it.  So if you're accelerating it at 2g coming up then you'd see twice the force as would normally be considered.  Granted that's just a cursory look over the problem you described.  I'll take some time later on to come up with a better thought on how to approach it, but if you have a picture/diagram explaining the outline and what you're wanting it would help me get oriented a little better.

Just out of curiosity are you applying this with a motion load analysis, or are you treating this as a static case at various instances/loads?

[vex]

So here's my best stab at your questions:

Will the pins mimic the bearing load?

The short answer is yes.  The load will translate through the various components of the assembly.  If you draw an FBD and make your cuts to isolate the pin from the eye you will see that the forces are necessary to translate between the three components.  The pin is just a solid mechanism to translate that force between the two links.  There's more detail here, but I don't think it's really necessary to go in to.

The results in the image seem about right to me?

Some results can be misleading.  Have you checked the convergence of the various results (stress, 1st, 3rd, displacement)?  If so, how does it look?  If they aren't converged then you have some cleaning up/refining to do to show it accurately.  If they did converge; great! You have a good idea of what forces and stresses you'll be seeing.  For me, I usually like to run a test case or two to verify that the results are accurate.  For instance I did a 'by-hand' calculation for a tow bitt and the stresses that would be seen (both bearing and bending).  When I ran the rest through Stress Analysis I had 0% difference between my hand calculations vs the FEA (it was something like 6547 psi vs 6540 psi).  If you start from that prospect it should help solidify the idea of what is accurate with your model and what is not.

As for the dynamic simulation: I'm not 100% sure it's necessary here.  It very well could be, but I'm not exactly sure that's what your big concern is.  If your concern is the failure of pins based on the dynamic loading you can treat it as a static load case--you'll just need to up your forces based on what load it will experience during that dynamic event (as previously discussed).  If you're concern is tied to a dynamic event/process, I can't really help you.  At least not in good faith.  Do the parts operate at high RPM or spontaneously undergo large changes in direction (acceleration)?  That's where you would see large dynamic loading. If your concern is fatigue loading you usually can get around that by increasing your factor of safety or incorporate some amount of additoinal force or material defect to account for it.

Does that help at all?

[chipwitch]

**** it!!  I tried to post a response, but looks like Firefox chocked on the request to send.  Locked me out of the forum.  Had to exit Firefox and restart.  Never seen that happen before.

Anyway... I need to go extract my laptop from the drywall and grab a bite to eat.  Be back shortly.

[chipwitch]

First off, "yes" you've been a big help.  I have a lot of confidence issues with using the analysis features.  You've provided me with some good info plus, and probably more importantly, many of your comments are inline with how I've envisioned the workflow, so at least I'm not too far off base.  I'll start with your previously unanswered post... like I mentioned, I had a response for it, but my browser choked when I hit the "send" button. 

Why doesn’t the rich text formatting work on this forum?…. Makes it hard to communicate. Hope you can follow this.

vvvvvvvvvvvvvvvvv

Sorry about that (my next response will take some time to think out and write), I ment to say slip fit no sliding.  That's a manual contact so there needs to either be a suppressed automatic contact, a manual contact made before you do an automatic, or decrease the size such that the gap is larger than the automatic threshold (or you can adjust the automatic threshold).

 ^^^^^^^^^^^^^^^^^^^

I know what a "slip fit" is but not as it pertains to the Stress Analysis Software.  Do you mean "shrink fit/no sliding?"  Are you conflating the Stress analysis with the Dynamic environment and talking about joints?  I know how you have the option for automatic joints in Dynamic area or manual and manual will reveal the standard joints, but I still don't know a "slip fit" there either.

vvvvvvvvvvvvvvvvv

As for dynamic simulations, that's a little outside my expertise with Inventor (i've dabbled with it, but not enough to give any advice or direction with).  From my perspective I would treat it as a worst case scenario: you mass*acceleration is going to be your force acting on it.  So if you're accelerating it at 2g coming up then you'd see twice the force as would normally be considered.  Granted that's just a cursory look over the problem you described.  I'll take some time later on to come up with a better thought on how to approach it, but if you have a picture/diagram explaining the outline and what you're wanting it would help me get oriented a little better.

^^^^^^^^^^^^^^^^^^^

I see you mentioned increasing the safety factor in your next post.  Basically, you're saying the same thing here.  I will be doing that too, but my reasoning for using the dynamic analysis is for extracting the FEA data from the time steps.  Not only is it more efficient, but the load at a joint in my linkage will change in magnitude and direction depending not only on the overall load of the real world assembly but also depending on the height the hitch is raised to (load's x, y and z components will obviolusly change) and most importantly, the linkage system is leveraged in different locations, joints acting as the fulcrum.  Think of a pantograph.  Calculations aren't impossible to do long hand, but if you have the software you spent 10 grand for, why not use it? 

 vvvvvvvvvvvvvvvvv

Just out of curiosity are you applying this with a motion load analysis, or are you treating this as a static case at various instances/loads?

 ^^^^^^^^^^^^^^^^^^^

I don't see much difference.  No matter what, it's still static.  The dynamic just finds the load equivalents and applies them. No?  Doing the motion load analyis is merely taking a snapshot of the positions and loads at a single point in time to be analyzed in FEA.

 vvvvvvvvvvvvvvvvv

Will the pins mimic the bearing load?

The short answer is yes.  The load will translate through the various components of the assembly.  If you draw an FBD and make your cuts to isolate the pin from the eye you will see that the forces are necessary to translate between the three components.  The pin is just a solid mechanism to translate that force between the two links.  There's more detail here, but I don't think it's really necessary to go in to.

 ^^^^^^^^^^^^^^^^^^^

When you say "cuts" I take that to mean you're using a split face or split body to isolate the pin from the eye?  Or is that something you can do to an FBD?  I don't remember that term with regard to FBDs?  I'm going to assume you were referring to the former...  I realize the forces will translate all the way through.  No contact can change that.  Put a 500 lb anvil on a table and the sum of the forces of the legs on the floor will equal the same.  But, my perception of the FEA tool is that the stress at the points of contact can be inaccurate (misleading at least) depending upon the contact used.  Bonded contact for example, transfers the load at the point of contact differently than say a sliding/no separation contact.  My concern isn't for the pin.  The pin is a means to an end for the sake of modeling.  We can disregard the modeling the stresses of the pin as far as I'm concerned, but the stress on the bearing surface AND the immediately surrounding area IS VERY important to me.  I want to know that my holes aren't too close to the edge and that tear out isn't going to be an issue.

 vvvvvvvvvvvvvvvvv

The results in the image seem about right to me?

Some results can be misleading.  Have you checked the convergence of the various results (stress, 1st, 3rd, displacement)?  If so, how does it look?  If they aren't converged then you have some cleaning up/refining to do to show it accurately.  If they did converge; great! You have a good idea of what forces and stresses you'll be seeing.  For me, I usually like to run a test case or two to verify that the results are accurate.  For instance I did a 'by-hand' calculation for a tow bitt and the stresses that would be seen (both bearing and bending).  When I ran the rest through Stress Analysis I had 0% difference between my hand calculations vs the FEA (it was something like 6547 psi vs 6540 psi).  If you start from that prospect it should help solidify the idea of what is accurate with your model and what is not.

 ^^^^^^^^^^^^^^^^^^^

Yes, I'm getting convergence when I ignore the pins.  Keep in mind, when I say "seems about right," I was referring to the way the stresses were being displayed at the bearing surfaces primarily.

 vvvvvvvvvvvvvvvvv

As for the dynamic simulation: I'm not 100% sure it's necessary here.  It very well could be, but I'm not exactly sure that's what your big concern is.  If your concern is the failure of pins based on the dynamic loading you can treat it as a static load case--you'll just need to up your forces based on what load it will experience during that dynamic event (as previously discussed).  If you're concern is tied to a dynamic event/process, I can't really help you.  At least not in good faith.  Do the parts operate at high RPM or spontaneously undergo large changes in direction (acceleration)?  That's where you would see large dynamic loading. If your concern is fatigue loading you usually can get around that by increasing your factor of safety or incorporate some amount of additoinal force or material defect to account for it.

 ^^^^^^^^^^^^^^^^^^^

I agree with the point about dynamic simulation being unnecessary.  But, I think it is more efficient.  Why not let it generate the time steps for multiple FEA models from one single dynamic model?  I believe it should be clear that I've now already addressed some of the points you make here... The pin isn't my concern.  It's pretty easy to calculate the strength of the pin.  But, I do want to see the stress on the female bearing surfaces caused by the pin.  I'm not really concerned with any kind of dynamic event/process per se.  I simply don't know what the loads will be at the individual joints and the dynamic simulation will reveal all the joints in all positions in short order (FEA export). 

Being that farm implements will be hanging off the hitch (and directly responsible for the lion's share of the load), it is also subject to intermittent, sudden side loads and even uploads.  That's the extent of the expected changes in acceleration.  Putting it in the dynamic environment to evaluate various conditions seemed like a good idea at the time.  As for increasing the safety factor... Well, how much?  Isn't the point of engineering to avoid WAGs?  Of course, I'll be adding plenty of safety factor as well! 

vvvvvvvvvvvvvvvvv

Does that help at all?

^^^^^^^^^^^^^^^^^^^

Yes, yes, yes, yes yes!  Can I accept all your posts as the solution?    I have sincerely appreciated your thoughtful responses.